1 / 54

CAM Systems & CNC Machine Overview - Lecture 3

CAM Systems & CNC Machine Overview - Lecture 3. Overview to Computer Aided Manufacturing - ENGR-2963 - Fall 2005 Class Manager - Sam Chiappone. History.

tamma
Télécharger la présentation

CAM Systems & CNC Machine Overview - Lecture 3

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. CAM Systems & CNC Machine Overview - Lecture 3 Overview to Computer Aided Manufacturing - ENGR-2963 - Fall 2005 Class Manager - Sam Chiappone

  2. History • 1955 - John Parsons and US Air Force define a need to develop a machine tool capable of machining complex and close tolerance aircraft parts with the same quality time after time (repeatability). MIT is the subcontractor and builds the machine for the project.

  3. History: Continued • 1959 - MIT announces Automatic Programmed Tools (APT) programming language • 1960 - Direct Numerical Control (DNC). This eliminates paper tape punch programs and allows programmers to send files directly to machine tools

  4. History: Continued • 1968 - Kearney & Trecker machine tool builders market first machining center • 1970’s - CNC machine tools & Distributed Numerical Control • 1980’s - Graphics based CAM systems introduced. Unix and PC based systems available

  5. History: Continued • 1990’s - Price drop in CNC technology • 1997 - PC- Windows/NT based “Open Modular Architecture Control (OMAC)” systems introduced to replace “firmware” controllers.

  6. Control Systems • Open-Loop Control • Stepper motor system • Current pulses sent from control unit to motor • Each pulse results in a finite amount of revolution of the motor001” is possible

  7. Control Systems • Open-Loop Limitations • Control unit “assumes” desired position is achieved • No positioning compensation • Typically, a lower torque motor • Open-Loop Advantages • Less complex, Less costly, and lower maintenance costs

  8. Control Systems • Closed-Loop Control • Variable DC motors - Servos • Positioning sensors -Resolvers • Feedback to control unit • Position information compared to target location • Location errors corrected

  9. Control Systems • Closed-Loop Advantages • DC motors have the ability to reverse instantly to adjust for position error • Error compensation allows for greater positional accuracy (.0001”) • DC motors have higher torque ranges vs.. stepper motors • Closed-loop limitations • Cost

  10. Three Basic Categories of Motion Systems • Point to Point - No contouring capability • Straight cut control - one axis motion at a time is controlled for machining • Contouring - multiple axis’s controlled simultaneously

  11. Three Basic Categories of Motion Systems

  12. CNC vs. NC Machine Tools • Computer Numerical Control (CNC) - A numerical control system in which the data handling, control sequences, and response to input is determined by an on-board computer system at the machine tool.

  13. CNC • Advantages • Increased Program storage capability at the machine tool • Program editing at the machine tool • Control systems upgrades possible • Option -resident CAM system at machine tool • Tool path verification

  14. NC • Numerical Control (NC) - A control system which primarily processes numeric input. Limited programming capability at the machine tool. Limited logic beyond direct input. These types of systems are referred to as “hardwire controls” and were popular from the 1950’s to 1970’s.

  15. Machining Centers • A machining center can be defined as a machine tool capable of: • Multiple operation and processes in a single set-up utilizing multiple axis • Typically has an automatic mechanism to change tools

  16. Machining Centers • Machine motion is programmable • Servo motors drive feed mechanisms for tool axis’s • Positioning feedback is provided by resolvers to the control system

  17. Machining Centers • Example - A turning center capable of OD turning, external treading, cross-hole drilling, engraving, and milling. All in machining is accomplished in one “set-up.” Machine may have multiple spindles.

  18. Machining Centers

  19. Programming Methods • Automatically Programmed Tools (APT) • A text based system in which a programmer defines a series of lines, arcs, and points which define the overall part geometry locations. These features are then used to generate a cutter location (CL) file.

  20. Programming Methods-APT • Developed as a joint effort between the aerospace industry, MIT, and the US Airforce • Still used today and accounts for about 5 -10% of all programming in the defense and aerospace industries

  21. Programming Methods-APT • Requires excellent 3D visualization skills • Capable of generating machine code for complicated part programs • 5 axis machine tools

  22. Programming Methods-APT • Part definition • P1=Point/12,20,0 • C1=Circle/Center,P1,Radius,3 • LN1=Line/C1. ATANGL,90 • Cutter Commands • TLRT,GORT/LN1.TANTO,C1 • GOFWD/C1,TANTO,L5

  23. Programming Methods-CAM • Computer Aided Machining (CAM) Systems • Graphic representation of the part • PC based • Integrated CAD/CAM functionality • “Some” built-in expertise • Speed & feed data based on material and tool specifications

  24. Programming Methods-CAM • Tool & material libraries • Tool path simulation • Tool path editing • Tool path optimization • Cut time calculations for cost estimating

  25. Programming Methods-CAM • Import / export capabilities to other systems • Examples: • Drawing Exchange Format (DXF) • Initial Graphics Exchange Standard (IGES)

  26. The Process CAD to NC File • Start with graphic representation of part • Direct input • Import from external system • Example DXF / IGES • 2D or 3D scan • Model or Blueprint (At this point you have a graphics file of your geometry)

  27. The Process CAD to NC File • Define cutter path by selecting geometry • Contours • Pockets • Hole patterns • Surfaces • Volume to be removed (At this point the system knows what you want to cut)

  28. The Process CAD to NC File • Define cut parameters • Tool information • Type, Rpm, Feed • Cut method • Example - Pocket mill zig-zag, spiral, inside-out • Rough and finish parameters (At this point the system knows how you want to cut the part)

  29. The Process CAD to NC File • Execute cutter simulation • Visual representation of cutter motion • Modify / delete cutter sequences (At this point the system has a “generic” cutter location (CL) file of the cut paths)

  30. The Process CAD to NC File • Post Processing • CL file to machine specific NC code • Filters CL information and formats it into NC code based on machine specific parameters • Work envelope • Limits - feed rates, tool changer, rpm’s, etc. • G & M function capabilities

  31. Output: NC Code • Numerical Control (NC) Language • A series of commands which “direct” the cutter motion and support systems of the machine tool.

  32. Output: NC Code • G-Codes (G00, G1, G02, G81) • Coordinate data (X,Y,Z) • Feed Function (F) • Miscellaneous functions (M13) • N - Program sequence number • T - Tool call • S - Spindle command

  33. Output: NC Code • NC Program Example • N01G90 G80 • N03 GOO T12 M06 • N05 GOO X0 Y0 Z.1 F10 S2500 M13 • N07 G1Z-.5 • N09 G02 X-10. I0J0F20 • N13 X0Y10 • N17 X10Y0 • N19 X0Y-10 • N21 X-10Y0 • N23 M2

  34. Example of CNC Programming • What What Must Be Done To Drill A Hole On A CNC Vertical Milling Machine

  35. Tool Home Top View 1.) X & Y Rapid To Hole Position Front View

  36. Top View 2.) Z Axis Rapid Move Just Above Hole 3.) Turn On Coolant 4.) Turn On Spindle .100” Front View

  37. Top View 5.) Z Axis Feed Move to Drill Hole Front View

  38. Top View 6.) Rapid Z Axis Move Out Of Hole Front View

  39. Top View 7.) Turn Off Spindle 8.) Turn Off Coolant 9.) X&Y Axis Rapid Move Home Front View

  40. Here’s The CNC Program! Tool At Home O0001 Top View N005 G54 G90 S600 M03 N010 G00 X1.0 Y1.0 N015 G43 H01 Z.1 M08 N020 G01 Z-.75 F3.5 N025 G00 Z.1 M09 N030 G91 G28 X0 Y0 Z0 Front View N035 M30

  41. Tool At Home O0001 Top View O0001 Number Assigned to this program Front View

  42. Tool At Home O0001 Top View N005 G54 G90 S600 M03 N005 Sequence Number G54 Fixture Offset G90 Absolute Programming Mode S600 Spindle Speed set to 600 RPM M03 Spindle on in a Clockwise Direction Front View

  43. O0001 Top View N005 G54 G90 S600 M03 N010 G00 X1.0 Y1.0 G00 Rapid Motion X1.0 X Coordinate 1.0 in. from Zero Y1.0 Y Coordinate 1.0 in. from Zero Front View

  44. O0001 Top View N005 G54 G90 S600 M03 N010 G00 X1.0 Y1.0 N015 G43 H01 Z.1 M08 G43 Tool Length Compensation H01 Specifies Tool length compensation Z.1 Z Coordinate .1 in. from Zero M08 Flood Coolant On Front View

  45. O0001 Top View N005 G54 G90 S600 M03 N010 G00 X1.0 Y1.0 N015 G43 H01 Z.1 M08 N020 G01 Z-.75 F3.5 G01 Straight Line Cutting Motion Z-.75 Z Coordinate -.75 in. from Zero F3.5 Feed Rate set to 3.5 in./min. Front View

  46. O0001 Top View N005 G54 G90 S600 M03 N010 G00 X1.0 Y1.0 N015 G43 H01 Z.1 M08 N020 G01 Z-.75 F3.5 N025 G00 Z.1 M09 Front View G00 Rapid Motion Z.1 Z Coordinate .1 in. from Zero M09 Coolant Off

  47. O0001 N005 G54 G90 S600 M03 Top View N010 G00 X1.0 Y1.0 N015 G43 H01 Z.1 M08 N020 G01 Z-.75 F3.5 N025 G00 Z.1 M09 N030 G91 G28 X0 Y0 Z0 G91 Incremental Programming Mode G28 Zero Return Command X0, Y0, Z0 X,Y,& Z Coordinates at Zero Front View

  48. O0001 Top View N005 G54 G90 S600 M03 N010 G00 X1.0 Y1.0 N015 G43 H01 Z.1 M08 N020 G01 Z-.75 F3.5 N025 G00 Z.1 M09 N030 G91 G28 X0 Y0 Z0 Front View N035 M30 M30 End of Program

  49. Output: NC Code - Canned Cycles

  50. CAD to NC Code

More Related